T2 Programming for 200 please Bob!

Hi Guys,

I'm stuck on a good way to program the od of this part. It looks kind of like a Tuba mouth piece with no hole though the stem. It's brass 1.5 od stock.

I'd love to use a groove-turn tool to do this, as it'd be damn simple, but I can't figure out how to get the machine to plunge in, traverse over, come out, do again deeper, etc.

Any advice is helpful!

Thanks,

Grant

I'm all thumbs when it comes to attachments....but I got it in there now.

Use Basic OD Turn & Part-Off . The print is poor but can make out basic shape. In Fact it looks a Lot similar to a part in the Mazak training course/

Thanks for the reply!

When I do a basic od and turn, even with a VNMG there's a part of the profile that does not get cut. It's at the base of the large od raius where it meets the .5" shaft.

Corner OUT only lets you choose a tool to get the unmachined portion of a square or radiused corner, but does not allow a shape like that.

Coming at it the other way with a left hand tool has a similar problem, but on the other end.

The idea I'm working with at this point is a groove to releive the .5 shaft most of the way, then cut with a left hand vnmg to get the result I want.

Any more ideas?

Thanks!

Grant

I would use a Kenametal Turn and Groove insert with a .007 corner radius. The profile should be easy enough to program and no cutter comp. Turn small diameter to big and part off.

It's not cutting it with the VNMG because it's physically impossible without cutting into the sphere. If you want to use a groove tool to do it teach it as a turning tool, offset width of groover. Or manually program it.

Midnight Machinist said:

View attachment 89553Hi Guys,

I'm stuck on a good way to program the od of this part. It looks kind of like a Tuba mouth piece with no hole though the stem. It's brass 1.5 od stock.

I'd love to use a groove-turn tool to do this, as it'd be damn simple, but I can't figure out how to get the machine to plunge in, traverse over, come out, do again deeper, etc.

Any advice is helpful!

Thanks,

Grant

Click to expand...

Piece-o-cake. I do this all the time.

Define as normal OD groove tool. Be sure to enter the exact width and radius of the grooving insert. For example say you are using .062" wide tool with .007" corner radius.

The old controls are not designed to use a groove tool as a turning tool, but it can be made to work.
Program the job as you would BAR OUT (not grooving cycle), but you need to adjust the geometry on the trailing Z side of the insert to account for the flat on the groove insert between the corner radii. In this case, .062 -.007 -.007 = .048".

The machine will automatically compensate for a full radius tool, but ignores the flat on this insert. Solution is to manually add .048" to the Z lengths on the trailing Z side of the geometry (only 3 dims, start of CHF, start and end of .484 rad.) and run the program with rough and finish tools. Lead side of geometry is unchanged.

The geo on the screen will look wrong, but when you run a simulation or trace, you will see the tool cut the geometry correctly.

The above is not necessary for turning ops with full radius groove inserts as they work fine.

This takes a few seconds to change the geo. Program the job manually? F that.

When I do a basic od and turn, even with a VNMG there's a part of the profile that does not get cut. It's at the base of the large od raius where it meets the .5" shaft.

Click to expand...

You could even rough the profile with the VNMG with correct geometry without a finish tool. Then on a second process, use the above method with CPY OUT rough and finish tools (or just a finish tool) to remove the uncut portion left from the previous VNMG tool. (process copy, adjust Z values and change tool info, done)

Perfect Philabuster!!

That's exactly what I was looking for.

I even bothered Mazak Applications for a while and they had no success.

Thank you!! I'll let you know how it goes!

Cheers,

Grant

My Machine does not seem to want to do this...

Hi Philabuster and Company.

Here are my relevant screens. I hope there's mistakes, that make the thing not want to work, but I think it should.

I've tried bar out reverse, where the grooving tool is called out as a left hand tool, and also as bar out regular, where the grooving tool is defined as a right hand tool.

Neither one works. I've shown what the tool path check does when it gets to what I had hoped was "magical bar out groove turn". I don't understand why it does that.

I suspect my machine may not be as smart as the regular issue QT15's as there's a few things that don't work (editing program while another one runs, etc.) that should.

I'm stumped!

Thanks again,

Grant

Philabuster said:

Piece-o-cake. I do this all the time.

Define as normal OD groove tool. Be sure to enter the exact width and radius of the grooving insert. For example say you are using .062" wide tool with .007" corner radius.

The old controls are not designed to use a groove tool as a turning tool, but it can be made to work.
Program the job as you would BAR OUT (not grooving cycle), but you need to adjust the geometry on the trailing Z side of the insert to account for the flat on the groove insert between the corner radii. In this case, .062 -.007 -.007 = .048".

The machine will automatically compensate for a full radius tool, but ignores the flat on this insert. Solution is to manually add .048" to the Z lengths on the trailing Z side of the geometry (only 3 dims, start of CHF, start and end of .484 rad.) and run the program with rough and finish tools. Lead side of geometry is unchanged.

The geo on the screen will look wrong, but when you run a simulation or trace, you will see the tool cut the geometry correctly.

The above is not necessary for turning ops with full radius groove inserts as they work fine.

This takes a few seconds to change the geo. Program the job manually? F that.



You could even rough the profile with the VNMG with correct geometry without a finish tool. Then on a second process, use the above method with CPY OUT rough and finish tools (or just a finish tool) to remove the uncut portion left from the previous VNMG tool. (process copy, adjust Z values and change tool info, done)

Click to expand...

The only reason I'd suggested manual programming is that if he was making thousands and thousands he'd probably want to have a better groove turning path then just using a bar out pass in one direction.

Sorry for double post but I'm in a hurry, shouldn't you have told the machine that it's a od turning tool? I've only done it in a t32 but u remember just telling it that I was using a turning tool with a ridiculously low angle. All you're other tool data's look weird as hell to me.

Don't do just a trace check do a full simulation.

Midnight Machinist said:

Hi Philabuster and Company.

Here are my relevant screens. I hope there's mistakes, that make the thing not want to work, but I think it should.

I've tried bar out reverse, where the grooving tool is called out as a left hand tool, and also as bar out regular, where the grooving tool is defined as a right hand tool.

Neither one works. I've shown what the tool path check does when it gets to what I had hoped was "magical bar out groove turn". I don't understand why it does that.

I suspect my machine may not be as smart as the regular issue QT15's as there's a few things that don't work (editing program while another one runs, etc.) that should.

I'm stumped!

Thanks again,

Grant

Click to expand...

Thank you for providing ALL of these screen shots along with the CAD sketch of the part. This was extremely helpful. I was able to re-create the exact toolpath as shown with the tool data you provided.

I then changed the tool data to my smaller grooving tool and it worked on your program. Hmmm...

Well, I figured out where the problem is at and how to avoid it.

Do not describe the groove tool deeper than .300" or machine pukes on toolpath. The groove tool depth is purely for visual reference on the Trace or Simulation screens, but obviously does something to mess up the works when trying to use as turning tool. Machine is probably thinking there is no way this long, skinny tool can be used as a turning tool and prevents such foolish actions.

The groove tool depth on the Tool File page does not limit or prevent the machine from cutting a groove deeper than as described here.

The described groove tool width is extremely important as is the tool's radius.

BTW, your altered Z values are correct to use with this groove tool. I guess my long winded explanation was helpful after all.

Issue about not able to edit program while running another job...

This is hit or miss for me and I have not tracked the real issue down exactly why just yet. I do know that I can always create a new program while machine is cutting chips. If I want to edit a program while running, I have found a way to make this happen. I create a new program and fill in the PNo0 line as normal. Then on 1st process, I simply copy the entire program I originally wanted to edit into my new program, done.

I can perform shape check on the part, but machine will not allow you to perform the toolpath check--unless, you first hit FEED HOLD, perform toolpath check, then when it is finished, go back to Trace screen and hit CYCLE START. This old computer can only calculate one toolpath at a time--it cannot cut parts and run toolpath check simultaneously.

Well done Philabuster!!!

That'll open up a whole new way to program for me!!

I feel like I'm only getting 60% of what the machine can do, the rest I do in a dumb way because I don't know any better.

I'll post a pic of the finished thing when I'm done so you can see what the fuss is about.

I'll have to fiddle with the create new program business later, first I gotta get these dang parts done!

Thank you again, very much for your help with this, Lyk31337 too! I love this place!

I'm certain you could teach the folks at Mazak a thing or two about the "legacy" machines...

Cheers,

Grant

Dang!!!! I wish I could get close to that 60%!!!

You're welcome.

I noticed the yellow line of the chuck barrier was showing up in your toolpath check graphic. This probably means you had to disable the barriers to get this part to run.

In order to electronically move the chuck back out of the way, go to the Program File page, cursor down to active work number (415) and cursor over to Chuck-Z field. Enter -5" and this will slide the chuck back 5" when you go to toolpath check or Trace screen. I do this on all programs that need soft jaws. This will also mean you can now run without cancelling the barriers.

If I am using hard jaws, I created the jaws in the jaw file page and call them up as Jaw 1 in the Program File and I enter the Chuck-Z value of -1.2". The way my machine is set up, this gives me about .100" clearance from my tool to the jaws until the machine triggers the chuck barrier. This is really handy to have if you are running multiple parts using the repeat function and offsetting the program in -Z each part. This keeps me from crashing into the jaws if I over calculate the number of parts I can get for a given stickout length of the bar.

I also want to show you guys a special tool description that literally disables the tool protection and will allow you to do damn near anything you want. This is really handy when programming full radius button tools and need the freedom to cut the part. The non-cut area of the part left from the VNMG in the original example above is due to machine only cutting the stock it can reach without wiping out the part. This safety zone around the tool is handy for most cases, but on some tools this becomes an obstacle.

Anyway, here it is. GNL EDG 3, 0 and enter correct tool radius of insert on Tool Data along with usual RH or LH tool and direction arrow. Again, this method needs to be used with caution.

The toolpath check will verify machine compensates correctly for tool radius, but now literally ignores everything else. This description can be used when profiling ANY shape being ID, OD or FCE cuts. The Trace graphics will look completely wrong for a given tool, but the machine will do EXACTLY whatever you see on the Trace screen.

I'm certain you could teach the folks at Mazak a thing or two about the "legacy" machines...

Click to expand...

Nice thing about Mazatrol is most of the trick stuff you will learn on the T-2 control is forward compatible for the newer controls. I say most of the stuff because I found a few tidbits here and there that were sacrificed along the way. The CPT-X and CPT-Z positions reduced to 2 place decimal kinda irked me when I was learning the T+ control in 1998. The TPC is the only thing I WISH I could retrofit on my T-3.

Midnight Machinist said:

I'd love to use a groove-turn tool to do this, as it'd be damn simple, but I can't figure out how to get the machine to plunge in, traverse over, come out, do again deeper, etc.

Click to expand...

I forgot to mention this but this grooving process would be better off to rough and finish in separate processes to avoid the groove tool trying to back turn the large 'wall' of the groove near the part off. Basically, just copy the process as is and remove the finish tool on first process and remove the roughing tool on the second process AND shorten up the Z dimension in line 4 to 1.76".

You can insert an additional line to the process (line 5) to greatly speed up the feedrate on the finish pass when the tool goes from the .5" dia to the 1.3" dia CPT-X position now that you are just cutting air.

5) LIN Start X.5, Start Z 1.76, Finish X1.3, Finish Z1.76, Surface Finish (SRF) 1

I have some small parts I rough the profile with a DNGP432 in one process, parts get drilled and bored, then the ODs get finished with the mentioned .062" wide R.007" Top Notch insert in a second process with altered Z values on trailing side. Actually, I use this dinky insert to finish turn the Z0 face, second face, three diameters, one 45° reverse angle with a R.060 and then use the same insert to then cut off the part and use it to barpull the 1/2" dia barstock.

To reduce sideload pressure on the tiny groove insert, I add a GRV OUT #0 process to use the insert to remove the .031" radius left from the DNGP432 on the second face before I run the finish profile and cutoff.

These parts will eventually get produced in high volumes on a swiss machine, but we are still in the R&D stage so I make batches of various sizes and shapes in a hundred or so lots for testing. I go from maxing out the swing on my 27 year old Mazak with the 15" jaws on the 8" chuck to barpulling 1/2" dia stock in hard jaws to make these parts that average about Ø.285 largest dia and .255" long.

Adjuisting my "mastery" of Mazatrol from 60% to 30%.

Well Sheeeeit Philabuster!

The more you write the more I realize I didn't know! If I were closer, I'd offer to be your apprentice for a week just to see how it's REALLY done with a T-2. As it is, I'll have to figure out some other way to help you in thanks for all the time and knowledge you've shared.

I will have to take a little while to absorb all this new information, but I am damn glad to find a way away around the SUPER slow retract on grooving (I thought it was a parameter error on my part), as well as everything else you've shared!

Anyhow, here's the proof of success, much to Philabuster's help.



Thanks again!!

Grant

Midnight Machinist said:

Well Sheeeeit Philabuster!

The more you write the more I realize I didn't know! If I were closer, I'd offer to be your apprentice for a week just to see how it's REALLY done with a T-2.

Click to expand...

It is SO much easier to show people stuff on the machine while you can converse back and forth real time. People usually learn real quick that asking me questions about my Mazak usually ends up in a several HOUR dissertation as to how many cool things this old girl can do. Often times, they end up doing this number trying to leave:

The info I shared in this thread would be easily shown while at the control in about 10 minutes. The nice thing is other people can reference this thread in the future (complete with the pictures) of how to get this old (but awesome!) control to work.

As it is, I'll have to figure out some other way to help you in thanks for all the time and knowledge you've shared.

Anyhow, here's the proof of success, much to Philabuster's help.

View attachment 89968

Thanks again!!

Grant

Click to expand...

This ^^^ is greatly appreciated. No additional thanks required. Definitely makes my long winded explanations worth it.

I would love to post pics of all the cool parts I have made over the years on my old Mazak, but not allowed, so I settled for an avatar of my 8" chuck sporting ridiculously oversized 15" jaws instead.

If Phil would just send me just 5% of his knowledge and skill I would be dancing in the street.